...
As for pull up resistor for the EEPROM... I have never done this and the PDF documentation for the Prop does not show a pull up on the EEPROM pins.
I'm looking at the QuickStart board and it does have pull up's on the EEPROM SCL/SDA.
A cursory glance around things shows pull-ups on the Activity Board, ASC+...
... pull ups on the BOE SPI MICRO_SD card lines
... pull ups on the BOE EEPROM SCL/SDA
....
I have never done this and the PDF documentation for the Prop does not show a pull up on the EEPROM pins.
Because, technically, the Propeller boot-loader violates the I2C spec by driving the SCL line high for a "1". There is always an SDA pull-up on Parallax boards because the external EEPROM -- following the spec -- does not drive the SDA line high for a "1". Most new Parallax boards include a pull-up on both (per spec). A resistor costs next to nothing and allows your project to work with I2C-compatible objects (i.e., objects that don't drive the SCL line high [like mine]).
I've attached schematics for design elements that I've used in several EFX-TEK (commercial) products. We're a tiny company and cannot afford to have anything go wrong. The button circuit is configured for active-high. If you prefer active-low you can swap the Vdd and Vss connections. The 10K is the pull-down; the series 3.3K (which allows for Vdd of 5v) helps protect the pin from static discharge.
And every time, I've felt a disturbance in the Force as the I2C spec is violated.
I'm pretty sure the Demo Board and PPDB are the only two Propeller boards Parallax sells which don't include a pull-up on the clock line. Jon already explained why the Propeller will still load properly without the second pull-up.
Hmm, that is some interesting information. I did not know that. I have always gone by the Prop Datasheet which does not show but 1 resistor on the EEPROM. That is an easy change to make before I get the boards ordered.
Other than that, is the board looking fair enough to finish up extending the pins to accessible locations then ordering or could I still improve on it? My biggest fear is that I will still have noise on the ADC which will cause strange readings. I think I will switch to using 12V through the RJ-45 connector as recommended which may open up other options for later modification if needed. Would a 7805 and this ( http://www.digikey.com/product-search/en?KeyWords=MCP1826S-3302E%2FAB-ND ) 3.3V regulator be ok to regulate the 12V down on the sensor board or should I go with a better 5V regulator?
On the program connector pin 4 sometimes there's a 10k pullup on the Tx. I guess you'll use this for loading only. If you wanted to do debug/development it might be nice to have the terminal window to print real time data.
From the Micorchip datasheet regarding the SDA/SCL suspects in question: "This is a bidirectional pin used to transfer addresses and data into and out of the device. It is an open drain terminal. Therefore, the SDA bus requires a pull-up resistor to VCC (typical 10 k for 100 kHz, 2 k for 400 kHz and 1 MHz)." Part Number 24AA256/24LC256/24FC256, the 8 pin DIP version. BUT what about SCL????
It would seem the SDA requires a pullup but not the SCL. But the prop setup for the I2C is "bus(SCL pin, SDA pin, modeX (0 or 1))". Mode 0 is open drain and Mode 1 is active drive high low. In the prop you may not be able to get open drain on the SDA without the same mode on the SCL. Hmmm?
I have a program that reads the status on I2C devices. I disconnected the SCL 10k pullup to 3.3V. It still worked. I connected the 10K to ground. It still worked. On a scope: 1) 10K->grnd- crisp 2V swing 2) no 10K pullup, swing with a little ringing 3) 10K to 3.3 = crisp full transition swing from 0v to 3.3V.
My 2 cents on the I2C : 10k = Good Idea on SCL even if it will works without it.
and send 12V from pin 1 of the 5V reg. The route would start on the GP side to break it away from the reg, then onto the dark side along the XBee upper socket and around the perimeter top and left and wrap around the pin 8 of the RJ45. Alternately you could run 12V to pin 2 or 7 and leave your options open.
This is based on your second layout. I don't have DipTrace so won't be able to look at your latest. Trace width is not so important because any voltage drop will be ignored by the regulator at the far end. 20mil should be fine.
" I can't seem to figure a way to route the 12V to the RJ-45 connector. And ideas? "
An often overlooked option would be a simple wire jumper. Provide for two holes and solder pads. It may not be aesthetically pure and pleasing but it gets the job done.
Well, I think I am about done. Thanks Hal for that recommendation. I did not think about running a wire from one part of the board to the next.
One other thing I am worried about is the RJ-45 connected directly to the prop with no protection. Since I will be running the ADC on a separate board at least 5 feet away, that is a good chance for voltage to cross directly into the Prop that is unfiltered. I don't want to risk the chance of popping the Prop with stray electricity. Is there something I could put in between the pin and the connector and still be able to reliably send data from the ADC and the Prop? And....Can the ADC send data to the Prop at that distance?
EDIT : For those who cannot see the changes through the file I uploaded, here is a screen shot. Please critique! Good, bad, or ugly. I would really like your input. I am hoping to nail this in one shot.
Well, I think I am about done. Thanks Hal for that recommendation. I did not think about running a wire from one part of the board to the next.
One other thing I am worried about is the RJ-45 connected directly to the prop with no protection. Since I will be running the ADC on a separate board at least 5 feet away, that is a good chance for voltage to cross directly into the Prop that is unfiltered. I don't want to risk the chance of popping the Prop with stray electricity. Is there something I could put in between the pin and the connector and still be able to reliably send data from the ADC and the Prop? And....Can the ADC send data to the Prop at that distance?
If in doubt then just allow for series resistors, the exact value you can determine at the time you load the board but I use 220R for general I/O or perhaps a much higher value if you know that it's always an input. In which case it doesn't hurt to allow for pullups too. I just use resistor arrays which especially in smt make a lot of sense as you squeeze four separate resistors into the same space as a 1206 and it costs about the same as a single resistor too. So here's a tip, allow for extra decoupling caps and resistors and pullups, even test points and connectors etc on your pcb design, then if you feel the need to load them you can, but if you don't allow for them then you can't. Doesn't cost anything extra to do this. I even bring out the I2C bus onto a 4-pin connector along with ground and 5V (or Vdd) just because I can and it can prove to be useful. But then again these signals are available on my standard 8-pin PropPlug compatible programming header which once again costs nothing.
I was trying to keep away from SMD components since I can't run to my local RadioShack and buy those in case I needed a different value. I have thousands of through hole resistors so I can salvage a bunch of those Going with SMD components, I could shink the size of the board tremendously but I have 5" to play with and once I get my hands inside the box, it is tough to test and probe things while it is in service. This board is pretty much set up for one specific thing and adding other I2C components is probably not going to happen. I am sure I could use this board for a bunch of things other than originally intended. Guess a few extra pads here and there will not hurt anything :P
I was trying to keep away from SMD components since I can't run to my local RadioShack and buy those in case I needed a different value. I have thousands of through hole resistors so I can salvage a bunch of those Going with SMD components, I could shink the size of the board tremendously but I have 5" to play with and once I get my hands inside the box, it is tough to test and probe things while it is in service. This board is pretty much set up for one specific thing and adding other I2C components is probably not going to happen. I am sure I could use this board for a bunch of things other than originally intended. Guess a few extra pads here and there will not hurt anything :P
Don't underestimate the value of a 4-pin I2C connector, even if you can't see how or when you will use it, it can get you out of a lot of design jams or simply prove useful for debugging. You could hang an LCD (even temporarily) off that port which under software could just be reporting its current status and variables etc, all without having to cart a laptop around. Then again I like to spit out that status info on the serial port all the time as my 8-pin connector allows me to plug in a serial Bluetooth module and all I need then is my phone or tablet to talk to it and see what's going on. I work with Tachyon which is fully interactive so I never get stuck scratching my head wondering what the software or hardware is doing, but still I allow for diagnostics, how much more so when you load a "binary blob" onto your board.
btw, the smt resnets were just a suggestion if you were so inclined as they make so much sense, and what's more I can gain different values from the "one component" in combinations. I used to do dual footprints for my TH and SMT components so you could make the choice when you assembled the board and doing so provides a good opportunity to gain experience with using smt. One again, doing so costs nothing but gives you a choice.
So I am about ready to zip up the gerber files and send this board off to be made but wanted to post the design one final time so I can get a second set of eyes on it. Since I am unsure what sensor setup I will be going with ATM so I added several pads next to the RJ45 connector so I can do whatever may be necessary there for whatever setup I decide to go with. I have tried to label everything that needs to be labeled so if there are any questions about components, please ask.
So I am about ready to zip up the gerber files and send this board off to be made but wanted to post the design one final time so I can get a second set of eyes on it. Since I am unsure what sensor setup I will be going with ATM so I added several pads next to the RJ45 connector so I can do whatever may be necessary there for whatever setup I decide to go with. I have tried to label everything that needs to be labeled so if there are any questions about components, please ask.
I am by no means a professional circuit designer but this is what has been pieced together from ideas / recommendations. Any input is appreciated!
Just quickly, the decoupler that you have just above the crystal is effectively useless, the ground for this and pin 24 are on opposite sides of the town, the long way around negates any benefits and yet you have room to connect to the ground close to pin 24. Another thing is check your design rules but the copper pour for the ground should be perfectly fine running between pads on the Prop as this will lead to a more effective ground.
As for the I2C connector if you are not sure what power you want to run then at least make it easy to connect 5V to it. BTW, I normally like to have the ground between signals and power just in case of a short so that I would run +5V, GND, then I2C. Do yourself a favor and use labels on the ID layer for some of those signals like you did on the main connector. Have you tried using combicons for the main connector? That way you get the benefit of screw terminals and the ease of a plug and socket. How about an outline around the XBee socket so it's quite clear which way it plugs in?
One thing though is that I really don't like the idea of those 470uF caps on the output of the regulator, it sure doesn't need them and the regs work a lot better without them but I see you have not provided separate 3.3V regs for the I/O pins on the main connector and the Prop when it costs nothing to allow for this in the first place. Above all, if you really want to keep the Prop happy, give it and it's immediate devices their own 3.3V supply. If you must use caps on the outputs of these then just use 10uF tantalums, never bother with electros here or big values either.
You could allow for a resistor in series with your cap isolation diode, the resistor helps filter out line transients and at the same time reduces the power-on surge when the caps charge. Allowing for a component even if it is not fitted or is shorted is quite common in designs, it saves having to have or to do another board.
Thank you for the tips! I have a feeling I need to switch a bunch of this to surface mount since I am running out of room for other things. The Xbee socket is a custom component and I did not take the time to draw the outline. I have a good idea of how big it is on the board since I have printed the design and put an Xbee on the paper to check for clearance.
I did not think about using a separate 3.3V regulator for other items separate from the Prop. I should probably do that... Could I also run the Xbee from the same 3.3V source as the Prop?
As for the 470uF caps... One is on the Xbee as I have read it could be required for when the Xbee transmits data. The second one was to act as a "filter" between the outgoing 3.3V to the sensors / limit switches. It may not be needed, but I added it in case I add an additional circuit board apart from the main board.
I have not heard of using a resistor in series with the diode + cap. Which side of the diode would this go on?
Thank you for the tips! I have a feeling I need to switch a bunch of this to surface mount since I am running out of room for other things. The Xbee socket is a custom component and I did not take the time to draw the outline. I have a good idea of how big it is on the board since I have printed the design and put an Xbee on the paper to check for clearance.
I did not think about using a separate 3.3V regulator for other items separate from the Prop. I should probably do that... Could I also run the Xbee from the same 3.3V source as the Prop?
As for the 470uF caps... One is on the Xbee as I have read it could be required for when the Xbee transmits data. The second one was to act as a "filter" between the outgoing 3.3V to the sensors / limit switches. It may not be needed, but I added it in case I add an additional circuit board apart from the main board.
I have not heard of using a resistor in series with the diode + cap. Which side of the diode would this go on?
Which side of the diode? (think about it)
The Xbee Pro can have a transmit current of 250ma but if a regulator can't handle that unless there is a big cap then there is something wrong with the design. The only reference I could find to this 470uF was from some Arduino forum when using it with a shield but that is because of a problem with the setup and perhaps the regulator itself is not able to handle the peaks. Don't just accept what anybody says, do your own research.
I can't see where you are running out of room though, that board has an air of spaciousness about it. It is very easy to wrangle the tracks/connectors on the adjacent pins to go around the decoupler cap near the crystal.
Have you tried running two thin separate 18ft wires to the power bank for the MCU power, and see if noise is gone.
It would act as inductor and voltage drop is not a big deal as you floor it down to 5v anyway.
Though you separate the Motor gnd and mcu gnd on the board, that is only 1inch then they share 18ft pipe with the chance of gnd bounce going back that little inch of separation.
P.S re-route NET29 the long way as to not block Ground from motor pin header from it's top part.
P.P.S
I would scrap the 4 way light sensor as you have a mcu it will know what angle do use depending on the date.
if you don't want to set dates, use a single light sensor to detect dusk & dawn that you do a running average over a week and depending on length of day you know what time of year it is and set angle to that.
I have no way of knowing the angle or degree the panels are facing since everything it is made from is scrap parts I had laying around and adapting precise angle / degree sensor would be quite difficult for me to achieve. With using the sensor, I know that I can fine tune the exact position of the panels to the sun regardless of the time of day or year.
One thought I did come up with is using USB instead of cat5. It may be a little more expensive, but USB cables are easy to come by. Most are shielded already. And....they have a range well over 5ft. Maybe I should look into that instead? This whole project has dwelled around noise getting to the sensor and causing unwanted results. If I can overcome this, the project will be complete.
In a previous post or thread, it was recommended to me to just put the ADC on the main board and run the IR sensors from the CAT5. I did some testing and this seems to be quite simple and able to be done now that I have rearranged the board. Since this thread keeps dragging on, I have spent the time to redesign and implement in what seems to be the easiest way for me.
I have added the additional 3.3V regulator as well but am a little worried the 5V regulator will not be able to keep up. The 5V regulator is a switching regulator capable of supplying 500ma. The 3.3V regulators I have selected are able to handle 1A. I highly doubt I will be drawing anywhere close to this and could possibly be over designing on the low voltage power supply. Any input?
You've got traces and ground plane under the antenna end of your XBee module. You might want to rotate it 90 degrees and hang that end over the edge of the board.
In the attached image you can see how I did this on a friend's project.
Ok, I rotated the XBee to have the antenna face up which may also come in handy if I change to the modules with the antenna adapter. All the traces should be connected now and I have a few questions...
On the Motor control, do I need pull downs on those 2 inputs per H-Bridge?
For the 3.3V supply to the sensors, is it ok to pull it from the Prop like I have it now?
I guess I am one of those who like to fabricate on the fly. I am in no way an engineer and write or draw it out on paper or design an entire schematic. Not trying to be rude or anything, but with the way I work, I design on the fly and try not to, IMO, waste time drawing it out and then have to basically redo the exact same thing I just got finished spending hours drawing out. A well commented PCB can act like a schematic unless it has thousands of parts which then a schematic may be needed. If I were to sit down and try to design an entire schematic for a PCB I would probably give up the first hour since I already know I will have to do this detailed work all over again.
For a project of this magnitude I think you're hurting yourself by NOT having a schematic. A schematic is much easier for others to review than a PCB. Once you're happy with the schematic, your PCB can be linked to it to make sure that all of your nets are connected.
In my projects (like the one I pictured above) it's an iterative process: I do the basic schematic without connecting anything to the Propeller. Then I place the components on the board. As I'm routing to the Propeller I pop back over to the schematic and make updates.
I have never messed with designing a schematic and am trying to see if I can bring over the components from the PCB to the Schematic editor. So far I have not been able to figure this out. I guess I have to start from scratch to design the schematic? It appears that each component has to be the same as what is on the PCB which is difficult to locate each and every one.... Anyone know if Diptrace has the option of converting a PCB to a Schematic?
When designing a PCB, I think of a breadboard and the components I will be using. I know I need a wire from one pin to a resistor so on the PCB, I run a trace the best route I can find. I continue to do this until I see all components of each "section" of the circuit are connected. To me, the breadboard is my schematic.
Anyone know if Diptrace has the option of converting a PCB to a Schematic?
No. It's kinda of one way street.
I used to design boards that I liked, (PCB layout), that I had to redo because of component changes. So I went back and did a schematic, and was able to swap some parts out with minimal problems. Plus a schematic is invaluable down the road, after you forgot all the stuff that when into the PCB.
Well Smile... So either I can order the boards and hope for the best (which I am pretty sure it will work), or I can spend countless hours trying to recreate the PCB as a schematic?
Comments
A cursory glance around things shows pull-ups on the Activity Board, ASC+...
... pull ups on the BOE SPI MICRO_SD card lines
... pull ups on the BOE EEPROM SCL/SDA
....
Because, technically, the Propeller boot-loader violates the I2C spec by driving the SCL line high for a "1". There is always an SDA pull-up on Parallax boards because the external EEPROM -- following the spec -- does not drive the SDA line high for a "1". Most new Parallax boards include a pull-up on both (per spec). A resistor costs next to nothing and allows your project to work with I2C-compatible objects (i.e., objects that don't drive the SCL line high [like mine]).
I've attached schematics for design elements that I've used in several EFX-TEK (commercial) products. We're a tiny company and cannot afford to have anything go wrong. The button circuit is configured for active-high. If you prefer active-low you can swap the Vdd and Vss connections. The 10K is the pull-down; the series 3.3K (which allows for Vdd of 5v) helps protect the pin from static discharge.
And every time, I've felt a disturbance in the Force as the I2C spec is violated.
I'm pretty sure the Demo Board and PPDB are the only two Propeller boards Parallax sells which don't include a pull-up on the clock line. Jon already explained why the Propeller will still load properly without the second pull-up.
Other than that, is the board looking fair enough to finish up extending the pins to accessible locations then ordering or could I still improve on it? My biggest fear is that I will still have noise on the ADC which will cause strange readings. I think I will switch to using 12V through the RJ-45 connector as recommended which may open up other options for later modification if needed. Would a 7805 and this ( http://www.digikey.com/product-search/en?KeyWords=MCP1826S-3302E%2FAB-ND ) 3.3V regulator be ok to regulate the 12V down on the sensor board or should I go with a better 5V regulator?
From the Micorchip datasheet regarding the SDA/SCL suspects in question: "This is a bidirectional pin used to transfer addresses and data into and out of the device. It is an open drain terminal. Therefore, the SDA bus requires a pull-up resistor to VCC (typical 10 k for 100 kHz, 2 k for 400 kHz and 1 MHz)." Part Number 24AA256/24LC256/24FC256, the 8 pin DIP version. BUT what about SCL????
It would seem the SDA requires a pullup but not the SCL. But the prop setup for the I2C is "bus(SCL pin, SDA pin, modeX (0 or 1))". Mode 0 is open drain and Mode 1 is active drive high low. In the prop you may not be able to get open drain on the SDA without the same mode on the SCL. Hmmm?
I have a program that reads the status on I2C devices. I disconnected the SCL 10k pullup to 3.3V. It still worked. I connected the 10K to ground. It still worked. On a scope: 1) 10K->grnd- crisp 2V swing 2) no 10K pullup, swing with a little ringing 3) 10K to 3.3 = crisp full transition swing from 0v to 3.3V.
My 2 cents on the I2C : 10k = Good Idea on SCL even if it will works without it.
www.techboneyard.com/home-stuff/Main-Board-V1.dip DipTrace V2.4.0.2
An often overlooked option would be a simple wire jumper. Provide for two holes and solder pads. It may not be aesthetically pure and pleasing but it gets the job done.
One other thing I am worried about is the RJ-45 connected directly to the prop with no protection. Since I will be running the ADC on a separate board at least 5 feet away, that is a good chance for voltage to cross directly into the Prop that is unfiltered. I don't want to risk the chance of popping the Prop with stray electricity. Is there something I could put in between the pin and the connector and still be able to reliably send data from the ADC and the Prop? And....Can the ADC send data to the Prop at that distance?
EDIT : For those who cannot see the changes through the file I uploaded, here is a screen shot. Please critique! Good, bad, or ugly. I would really like your input. I am hoping to nail this in one shot.
If in doubt then just allow for series resistors, the exact value you can determine at the time you load the board but I use 220R for general I/O or perhaps a much higher value if you know that it's always an input. In which case it doesn't hurt to allow for pullups too. I just use resistor arrays which especially in smt make a lot of sense as you squeeze four separate resistors into the same space as a 1206 and it costs about the same as a single resistor too. So here's a tip, allow for extra decoupling caps and resistors and pullups, even test points and connectors etc on your pcb design, then if you feel the need to load them you can, but if you don't allow for them then you can't. Doesn't cost anything extra to do this. I even bring out the I2C bus onto a 4-pin connector along with ground and 5V (or Vdd) just because I can and it can prove to be useful. But then again these signals are available on my standard 8-pin PropPlug compatible programming header which once again costs nothing.
Don't underestimate the value of a 4-pin I2C connector, even if you can't see how or when you will use it, it can get you out of a lot of design jams or simply prove useful for debugging. You could hang an LCD (even temporarily) off that port which under software could just be reporting its current status and variables etc, all without having to cart a laptop around. Then again I like to spit out that status info on the serial port all the time as my 8-pin connector allows me to plug in a serial Bluetooth module and all I need then is my phone or tablet to talk to it and see what's going on. I work with Tachyon which is fully interactive so I never get stuck scratching my head wondering what the software or hardware is doing, but still I allow for diagnostics, how much more so when you load a "binary blob" onto your board.
btw, the smt resnets were just a suggestion if you were so inclined as they make so much sense, and what's more I can gain different values from the "one component" in combinations. I used to do dual footprints for my TH and SMT components so you could make the choice when you assembled the board and doing so provides a good opportunity to gain experience with using smt. One again, doing so costs nothing but gives you a choice.
If you have the latest version of DipTrace, you can download the source file here : http://www.techboneyard.com/home-stuff/Main-Board-V1.dip
I am by no means a professional circuit designer but this is what has been pieced together from ideas / recommendations. Any input is appreciated!
Just quickly, the decoupler that you have just above the crystal is effectively useless, the ground for this and pin 24 are on opposite sides of the town, the long way around negates any benefits and yet you have room to connect to the ground close to pin 24. Another thing is check your design rules but the copper pour for the ground should be perfectly fine running between pads on the Prop as this will lead to a more effective ground.
As for the I2C connector if you are not sure what power you want to run then at least make it easy to connect 5V to it. BTW, I normally like to have the ground between signals and power just in case of a short so that I would run +5V, GND, then I2C. Do yourself a favor and use labels on the ID layer for some of those signals like you did on the main connector. Have you tried using combicons for the main connector? That way you get the benefit of screw terminals and the ease of a plug and socket. How about an outline around the XBee socket so it's quite clear which way it plugs in?
One thing though is that I really don't like the idea of those 470uF caps on the output of the regulator, it sure doesn't need them and the regs work a lot better without them but I see you have not provided separate 3.3V regs for the I/O pins on the main connector and the Prop when it costs nothing to allow for this in the first place. Above all, if you really want to keep the Prop happy, give it and it's immediate devices their own 3.3V supply. If you must use caps on the outputs of these then just use 10uF tantalums, never bother with electros here or big values either.
You could allow for a resistor in series with your cap isolation diode, the resistor helps filter out line transients and at the same time reduces the power-on surge when the caps charge. Allowing for a component even if it is not fitted or is shorted is quite common in designs, it saves having to have or to do another board.
I did not think about using a separate 3.3V regulator for other items separate from the Prop. I should probably do that... Could I also run the Xbee from the same 3.3V source as the Prop?
As for the 470uF caps... One is on the Xbee as I have read it could be required for when the Xbee transmits data. The second one was to act as a "filter" between the outgoing 3.3V to the sensors / limit switches. It may not be needed, but I added it in case I add an additional circuit board apart from the main board.
I have not heard of using a resistor in series with the diode + cap. Which side of the diode would this go on?
Which side of the diode?
The Xbee Pro can have a transmit current of 250ma but if a regulator can't handle that unless there is a big cap then there is something wrong with the design. The only reference I could find to this 470uF was from some Arduino forum when using it with a shield but that is because of a problem with the setup and perhaps the regulator itself is not able to handle the peaks. Don't just accept what anybody says, do your own research.
I can't see where you are running out of room though, that board has an air of spaciousness about it. It is very easy to wrangle the tracks/connectors on the adjacent pins to go around the decoupler cap near the crystal.
It would act as inductor and voltage drop is not a big deal as you floor it down to 5v anyway.
Though you separate the Motor gnd and mcu gnd on the board, that is only 1inch then they share 18ft pipe with the chance of gnd bounce going back that little inch of separation.
P.S re-route NET29 the long way as to not block Ground from motor pin header from it's top part.
P.P.S
I would scrap the 4 way light sensor as you have a mcu it will know what angle do use depending on the date.
if you don't want to set dates, use a single light sensor to detect dusk & dawn that you do a running average over a week and depending on length of day you know what time of year it is and set angle to that.
One thought I did come up with is using USB instead of cat5. It may be a little more expensive, but USB cables are easy to come by. Most are shielded already. And....they have a range well over 5ft. Maybe I should look into that instead? This whole project has dwelled around noise getting to the sensor and causing unwanted results. If I can overcome this, the project will be complete.
The Diptrace file is here : http://www.techboneyard.com/home-stuff/Main-Board-V1-1.dip
In a previous post or thread, it was recommended to me to just put the ADC on the main board and run the IR sensors from the CAT5. I did some testing and this seems to be quite simple and able to be done now that I have rearranged the board. Since this thread keeps dragging on, I have spent the time to redesign and implement in what seems to be the easiest way for me.
I have added the additional 3.3V regulator as well but am a little worried the 5V regulator will not be able to keep up. The 5V regulator is a switching regulator capable of supplying 500ma. The 3.3V regulators I have selected are able to handle 1A. I highly doubt I will be drawing anywhere close to this and could possibly be over designing on the low voltage power supply. Any input?
In the attached image you can see how I did this on a friend's project.
On the Motor control, do I need pull downs on those 2 inputs per H-Bridge?
For the 3.3V supply to the sensors, is it ok to pull it from the Prop like I have it now?
Any other recommendations?
Updated Diptrace file : http://www.techboneyard.com/home-stuff/Main-Board-V1-1.dip
Post #36
In my projects (like the one I pictured above) it's an iterative process: I do the basic schematic without connecting anything to the Propeller. Then I place the components on the board. As I'm routing to the Propeller I pop back over to the schematic and make updates.
It's been to norm since PCB's where invented:
http://www.radio-electronics.com/info/electronics-design/pcb/pcb-design-layout-process.php
As Jon said, it helps to make sure all you nets are connected correctly .
When designing a PCB, I think of a breadboard and the components I will be using. I know I need a wire from one pin to a resistor so on the PCB, I run a trace the best route I can find. I continue to do this until I see all components of each "section" of the circuit are connected. To me, the breadboard is my schematic.
No. It's kinda of one way street.
I used to design boards that I liked, (PCB layout), that I had to redo because of component changes. So I went back and did a schematic, and was able to swap some parts out with minimal problems. Plus a schematic is invaluable down the road, after you forgot all the stuff that when into the PCB.
I start now with schematic only.